Collaborative
Solutions Inc
Solutions
An ANSYS Support Distributor
Date Memo Status
November 12, 1999 Internal and External
From Memo Number
S. Imaoka STI45:000509C
Subject
ANSYS Tip of the Week: Conversion of Piezoelectric Material Data
1. Introduction:
1. Introduction:
1. Introduction:
1. Introduction:
Conversion of material properties of piezoelectric ceramics (such as PZT) has caused many users
confusion because of the difference between manufacturer-supplied data and the format required by
ANSYS. This memo hopes to clarify this point and to provide users with information on conversion
routines.
Section 2 outlines the general constitutive equations and provides a framework for the following
discussion. Sections 3-6 cover converting manufacturer s data to ANSYS data for the stiffness matrix,
dielectric constants, and piezoelectric constants.
2. Background Information:
2. Background Information:
2. Background Information:
2. Background Information:
Before proceeding to conversion routines, the basic constitutive relationship of piezoelectric
materials will be outlined. Some notation may be non-standard, although the author has tried to
keep consistent with notation in published data as well as Ch. 11 of the ANSYS Theory Manual.
T = mechanical stress
S = mechanical strain
D = electric displacement (also referred to in ANSYS as electric flux density)
E = electric field
The above notation (all capital letters) is used for both variables (vectors) and superscript
notation indicating evaluation of properties.
The constitutive relationship usually given by manufacturers or published data/reports is in the
following form:
E
{S}= [s ]{T}+ [d]{E}
Eqns. 1 & 2
T
{D}= [d]t {T}+[µ ]{E}
where
{T}= stress vector (six components x, y, z, yz, xz, xy)
{S}= strain vector (six components x, y, z, yz, xz, xy)
{D}= electric displacement vector (three components x, y, z)
{E}= electric field vector (three components x, y, z)
E
[s ]= compliance matrix evaluated at constant electric field, i.e. short circuit
[d] = piezoelectric matrix relating strain/electric field
t
[d] = piezoelectric matrix relating strain/electric field (transposed)
T
[µ ]= dielectric matrix evaluated at constant stress, i.e. mechanically free
2303 W. 190th St " Redondo Beach, CA 90278
310.896.1230 " FAX [phone] " http://www.csi-ansys.com
Collaborative
Solutions Inc
Solutions
An ANSYS Support Distributor
On the other hand, ANSYS requires data in the following form (taken from Equation 11.1-1 in the
ANSYS Theory Manual):
E
{T} = [c ]{S}- [e]{E}
Eqns. 3 & 4
t S
{D} = [e] {S}+[µ ]{E}
where
{T}= stress vector (six components x, y, z, xy, yz, xz)
{S}= strain vector (six components x, y, z, xy, yz, xz)
{D}= electric displacement vector (three components x, y, z)
{E}= electric field vector (three components x, y, z)
E
[c ]= stiffness matrix evaluated at constant electric field, i.e. short circuit
[e] = piezoelectric matrix relating stress/electric field
t
[e] = piezoelectric matrix relating stress/electric field (transposed)
S
[µ ]= dielectric matrix evaluated at constant strain, i.e. mechanically clamped
In order to convert the manufacturer s data presented in the form of Equations 1 & 2 to ANSYS
notation (Equations 3 & 4), Equation 1 needs to be based on stress rather than strain. The following
manipulations can be performed:
E
{S}= [s ]{T}+ [d]{E}
E
[s ]{T}= {S}-[d]{E} Eqns. 5-7
-1 -1
E E
{T}= [s ] {S}-[s ] [d]{E}
Since Equation 2 relates electric displacement to strain rather than stress, Equation 7 can then be
plugged back into Equation 2:
t T
{D}= [d] {T}+[µ ]{E}
-1 -1
t E T
ëÅ‚ E
{D}= [d] [s ] {S}-[s ] [d]{E}öÅ‚ +[µ ]{E} Eqns. 8-10
ìÅ‚ ÷Å‚
íÅ‚ Å‚Å‚
-1 -1
t E ëÅ‚ T t E
{D}= [d] [s ] {S}+ [µ ]-[d] [s ] [d]öÅ‚{E}
ìÅ‚ ÷Å‚
íÅ‚ Å‚Å‚
Upon comparison of Equation 7 & 10 with Equations 3 & 4, one can obtain the relationship
between manufacturer-supplied data and ANSYS-required values:
-1
E E
[c ]= [s ]
-1
S T E
[µ ]= [µ ]- [d]t[s ] [d] Eqns. 11-13
-1 -1
E E
[e] = [s ] [d] = [d]t[s ]
These equations will form the basis of the conversion routines discussed shortly. Note that the
manufacturer s data has mechanical vector in the form {x, y, z, yz, xz, xy} whereas ANSYS s
mechanical vector is in the form {x, y, z, xy, yz, xz}.
2303 W. 190th St " Redondo Beach, CA 90278
310.896.1230 " FAX [phone] " http://www.csi-ansys.com
Collaborative
Solutions Inc
Solutions
An ANSYS Support Distributor
3. Stiffness/Compliance Matrix:
3. Stiffness/Compliance Matrix:
3. Stiffness/Compliance Matrix:
3. Stiffness/Compliance Matrix:
There are three ways in which a user can input stress-strain data. One can use MP commands to
specify orthotropic material properties (EX, NUXY, GXY). Otherwise, a user can input an
anisotropic elastic matrix with TB,ANEL. At 5.6, the TBOPT field of the TB command controls
whether this is read as a stiffness or compliance matrix.1
Assuming polarization in the 3-axis (z-axis), one can  map manufacturer data to ANSYS data to
generate a compliance matrix:
E E E
îÅ‚s11 s12 s13 0 0 0 Å‚Å‚
ïÅ‚ śł
E E
s11 s13 0 0 0
ïÅ‚ śł
E
ïÅ‚ śł
-1
s33 0 0 0
E E
[s ]= [c ] = ïÅ‚ śł
E
s66 0 0
ïÅ‚ śł
ïÅ‚ E śł
s44 0
ïÅ‚ śł
E
ïÅ‚ śł
s44 ûÅ‚
ðÅ‚
E E E E
If s66 is not available, it can be determined from s66 = 2(s11 - s12).2 Note that if the user wants to
-1
E E
input stiffness matrix, he/she must calculate [c ]= [s ] . The user will need to do this to calculate
the other constants as noted in subsequent sections. The user can invert the compliance matrix in
Microsoft Excel using the MINVERSE function. For the TB,ANEL command, either matrix (stiffness
matrix or compliance matrix) can be input.
To input this data as compliance, the user can issue the following commands:
TB,ANEL,1,1,,1 ! Material #1, 1 TEMP, TBOPT=1 for compliance input
TBDATA, 1,se11,se12,se13 ! Input first row
TBDATA, 7,se11,se13 ! Input second row
TBDATA,12,se33 ! Input third row
TBDATA,16,se66 ! Input fourth row
TBDATA,19,se44 ! Input fifth row
TBDATA,21,se44 ! Input sixth row
One needs to replace all values of se12 above with appropriate numerical values of compliance.
On the other hand, to input this data as stiffness, the user can issue the following commands:
TB,ANEL,1,1,,0 ! Material #1, 1 TEMP, TBOPT=0 for stiffness input
TBDATA, 1,ce11,ce12,ce13 ! Input first row
TBDATA, 7,ce11,ce13 ! Input second row
TBDATA,12,ce33 ! Input third row
TBDATA,16,ce66 ! Input fourth row
TBDATA,19,ce44 ! Input fifth row
TBDATA,21,ce44 ! Input sixth row
One needs to replace all values of ce12 above with appropriate numerical values of stiffness, as
calculated by the inverse of the compliance matrix (using either mathematics/matrix programs such
as MATLAB or Mathcad or spreadsheet programs such as Excel, as mentioned above).
1
At 5.5 and prior, the compliance/stiffness matrix with TB,ANEL was controlled with a KEYOPT(2) setting for SOLID5/98 and
KEYOPT(6) for PLANE13
2(1 +½ )
1
xy
2 E E E
s66 = = = 2(s11 - s12)
Gxy Ex
2303 W. 190th St " Redondo Beach, CA 90278
310.896.1230 " FAX [phone] " http://www.csi-ansys.com
Collaborative
Solutions Inc
Solutions
An ANSYS Support Distributor
An alternative method instead of using TB,ANEL is to use MP commands. Assuming polarization in
the 3-axis (z-axis), the user can also convert manufacturer data to ANSYS data. Recall from Equation
2.1-4 in the ANSYS Theory Manual:
1 Ex xy y xz
îÅ‚ -½ E -½ Ez 0 0 0
Å‚Å‚
ïÅ‚ śł
1 E -½ Ez 0 0 0
y yz
ïÅ‚ śł
ïÅ‚ śł
-1 1 Ez 0 0 0
-1 E E
[D] = [s ]= [c ] =
ïÅ‚ śł
1 Gxy 0 0
ïÅ‚ śł
ïÅ‚ śł
1 Gyz 0
ïÅ‚ śł
1 Gxz
ïÅ‚ śł
ðÅ‚ ûÅ‚
Using the above relationship, one can input the stiffness via orthotropic MP commands as follows:
1
EX = = EY
E
s11
1
EZ =
E
s33
1 1
GXY = =
E E E
s66 2(s11 - s12)
1
GYZ = = GXZ
E
s44
E
s12
NUXY = -
E
s11
E
s13
NUYZ = - = NUXZ
E
s33
To input this data, one can issue the following commands:
MP,EX ,1,1/se11 ! Material #1, Elastic modulus
MP,EY ,1,1/se11
MP,EZ ,1,1/se33
MP,NUXY,1,-se12/se11 ! minor Poisson s ratio
MP,NUYZ,1,-se13/se33
MP,NUXZ,1,-se13/se33
MP,GXY ,1,1/se66 ! Shear modulus
MP,GYZ ,1,1/se44
MP,GXZ ,1,1/se44
One needs to replace all values of se12 above with appropriate numerical values of compliance.
2303 W. 190th St " Redondo Beach, CA 90278
310.896.1230 " FAX [phone] " http://www.csi-ansys.com
Collaborative
Solutions Inc
Solutions
An ANSYS Support Distributor
4. Permittivity Matrix:
4. Permittivity Matrix:
4. Permittivity Matrix:
4. Permittivity Matrix:
The permittivity matrix evaluated at constant strain is input into ANSYS. Oftentimes,
manufacturers data has permittivity evaluated at constant stress, so conversion is necessary.
As noted in Equation 12, one can calculate the dielectric constants based on constant strain from
the following relationship:
-1
S T E
[µ ]= [µ ]- [d]t[s ] [d]
After evaluating Equation 12 above, the user can input permittivity. The permittivity matrix has
only diagonal terms:
S S
îÅ‚µ11 0 0 Å‚Å‚ îÅ‚K11 0 0 Å‚Å‚
ïÅ‚ śł ïÅ‚ śł
S S S
[µ ]= µ11 0 = µo K11 0
ïÅ‚ śł ïÅ‚ śł
S S
ïÅ‚ śł ïÅ‚
µ33 K33 śł
ðÅ‚ ûÅ‚ ðÅ‚ ûÅ‚
S
µ11
S
where K11 = is relative permittivity.
µo
T
In ANSYS, although the user has the choice of inputting permittivity as an absolute value µ33 or
T
relative value K33 , starting from 5.4, the relative value is the recommended choice. Assuming
polarization in the 3-axis (z-direction), this can be input with the MP commands as follows:
EMUNIT,EPZRO,8.85e-12 ! Define free-space permittivity
MP,PERX,1,reps11 ! Material #1
MP,PERY,1,reps11
MP,PERZ,1,reps33
One should replace all values of reps33 above with appropriate numerical values of relative
permittivity.3
5. Density Input:
5. Density Input:
5. Density Input:
5. Density Input:
Density needs no conversion. It is input with the MP command as follows:
MP,DENS,1,dens ! Material #1
One needs to replace the value of dens above with the appropriate numerical value of density.
3
As noted above, the user has the option of inputting relative or absolute permittivity. Any small value (<1) will be automatically
recognized as absolute permittivity by ANSYS, so the user does not need to take any special action.
2303 W. 190th St " Redondo Beach, CA 90278
310.896.1230 " FAX [phone] " http://www.csi-ansys.com
Collaborative
Solutions Inc
Solutions
An ANSYS Support Distributor
6. Piezoelectric Constant Matrix:
6. Piezoelectric Constant Matrix:
6. Piezoelectric Constant Matrix:
6. Piezoelectric Constant Matrix:
Usually, manufacturers data has [d], which relates mechanical strain to electric field. However,
ANSYS requires [e], relating mechanical stress to electric field, so conversion is necessary.
Note from Equation 13 above, a relationship between [e] and [d] is established as follows:
-1 -1
E E
[e] = [s ] [d]= [d]t[s ]
where, assuming polarization in the 3-axis (z-direction) and symmetry in the unpolarized directions
( d32 = d31 and d24 = d15 ):
îÅ‚ 0 0 0 0 0 d15 Å‚Å‚
t ïÅ‚ śł
[d] = 0 0 0 0 d15 0
ïÅ‚ śł
ïÅ‚d31 d31 d33 0 0 0 śł
ðÅ‚ ûÅ‚
Recall from the above discussions that manufacturers data assumes the mechanical vector as {x, y, z,
yz, xz, xy} corresponding to {1, 2, 3, 4, 5, 6} indexes. Row 4 needs to be shifted to Row 5, and,
similarly, Row 5 Row 6, Row 6 Row 4. Hence, d15 and d24 are shifted one across.
-1
E E
The user can use this matrix with [s ] = [c ] to evaluate [e] (with 4, 5, 6 rows properly
modified), which will become:
îÅ‚ 0 0 e31 Å‚Å‚
ïÅ‚
0 0 e31 śł
ïÅ‚ śł
ïÅ‚ śł
0 0 e33
[e]=
ïÅ‚ śł
0 0 0
ïÅ‚ śł
ïÅ‚ śł
0 e15 0
ïÅ‚ śł
ïÅ‚e15 0 0 śł
ðÅ‚ ûÅ‚
To input this data, one can issue the following commands:
TB,PIEZ,1 ! Material #1, piezo matrix
TBDATA, 3,e31 ! Input first row
TBDATA, 6,e31 ! Input second row
TBDATA, 9,e33 ! Input third row
TBDATA,14,e15 ! Input fifth row
TBDATA,16,e15 ! Input sixth row
One needs to replace all values of e33 above with appropriate numerical values of piezo constants.
2303 W. 190th St " Redondo Beach, CA 90278
310.896.1230 " FAX [phone] " http://www.csi-ansys.com
Collaborative
Solutions Inc
Solutions
An ANSYS Support Distributor
7. Conclusion & Future Work:
7. Conclusion & Future Work:
7. Conclusion & Future Work:
7. Conclusion & Future Work:
This memo provided background information on the constitutive laws of piezoelectric ceramics,
both in manufacturer-supplied form as well as ANSYS notation. Sections 3-6 develop the equations
needed to convert material data to a form acceptable for use with ANSYS.
The attached Excel worksheet contains conversion routines to provide the user with a simple
way to produce material library data with the poling direction in either the z- or y-directions. Export
the sheet as CSV (comma-separated text), and this can be directly input into ANSYS. Sample material
properties are provided as well. Note that the author makes no guarantee or assumes no liability for
any data in the Excel worksheet.
John Thompson at ANSYS Technical Support has also issued a similar memo and a very useful
PIEZMAT macro to facilitate conversion of data. CSI or the author of this document can be
contacted to obtain this macro and document.
In the future, the author may add a separate document for conversion of piezoelectric material
properties if the data is assuming the constitutive equations written in terms of strain and electric
field (i.e., if one has the analogous [g] coefficients instead of [d] matrix). 2D material definition will
also be added (i.e., change poling direction to y-axis).
__________________________
Sheldon Imaoka
Engineering Consultant
310.896.1230 x103
2303 W. 190th St " Redondo Beach, CA 90278
310.896.1230 " FAX [phone] " http://www.csi-ansys.com